About ALE Adaptive Meshing

In problems where large deformation is anticipated the improved mesh quality resulting from adaptive meshing can prevent the analysis from terminating as a result of severe mesh distortion. In these situations you can use adaptive meshing to obtain faster, more accurate, and more robust solutions than with pure Lagrangian analyses.

Adaptive meshing is particularly effective for simulations of metal forming processes such as forging, extrusion, and rolling because these types of problems usually involve large amounts of nonrecoverable deformation. Because the final shape of the product can be drastically different from the original shape, a mesh that is optimal for the original product geometry can become unsuitable in later stages of the process when large material deformation leads to severe element distortion and entanglement. Element aspect ratios can also degrade in zones with high strain concentrations. Both of these factors can lead to a loss of accuracy, a reduction in the size of the stable time increment, or even termination of the problem.

You can use adaptive meshing to enable acoustic domain meshes to follow the large deformations of the bounding structure. In other applications you can use adaptive meshing and adaptive mesh constraints to model arbitrarily large amounts of ablation of material away from the domain.

Adaptive meshing of acoustic regions greatly extends the utility of acoustic analysis procedures. Abaqus can be used to model the response of a coupled structural-acoustic system subjected to structural preloads. By default, the structural-acoustic calculations are based on the original configuration of the acoustic domain. This approximation is adequate as long as the boundary between the fluid and structure does not experience large deformation during application of the preload. However, when the geometry of the acoustic domain changes significantly as a result of structural loading, the original acoustic configuration must be updated. An example is the interior cavity of a tire subjected to inflation, rim mounting, and footprint pressure loads.

The acoustic elements in Abaqus do not have mechanical behavior and, therefore, cannot model the deformation of the fluid when the structure undergoes large deformation. Abaqus/Standard solves the problem of computing the current configuration of the acoustic domain by periodically creating a new acoustic mesh that uses the same topology as the original mesh but with the nodal locations adjusted so that the deformation of the structural-acoustic boundary does not lead to severe distortion of the acoustic elements.

The geometric changes associated with the new acoustic mesh are then taken into account in a subsequent coupled structural-acoustic analysis. However, it is assumed that the material properties of the fluid, such as the density, do not change as a result of mesh smoothing.

Adaptive meshing can also model effects of ablation, or wear, by enabling you to define boundary mesh motions independent of the underlying material motion. An example is the wearing of a tire during its life, an effect that can significantly affect the performance of the structure.

Adaptive meshing in Abaqus/Explicit is designed to handle a large variety of problem classes, and employs a variety of smoothing methods, with controls that you can use to tailor the adaptivity to specific problems. The Abaqus/Explicit implementation allows you to do the following:

• to create entirely Eulerian models;

• to improve the quality of the mesh initially, before deformation begins; and

• to define tracer particles, which enable tracking and output of material-based results quantities.

Adaptive meshing in Abaqus/Standard uses a single smoothing algorithm that works well for structural acoustic analyses and the modeling of ablation processes. The Abaqus/Standard implementation of adaptive meshing has the following limitations:

• Initial mesh sweeps cannot be used to improve the quality of the initial mesh definition.

• The method is not intended to be used in general classes of large-deformation problems, such as bulk forming.

• Diagnostics capabilities are currently limited.

In this example a well-lubricated rigid die of sinusoidal shape moves down to deform a blank of rectangular cross-section (see Figure 1).

Figure 1. A blank and a sinusoidal die.

The indentation depth is 80% of the original blank thickness. Material extrudes upward and outward (radially) as the blank is indented. The die is modeled with an analytical rigid surface, and the blank is modeled with axisymmetric continuum elements in a regular mesh configuration. The blank is assumed to have elastic-plastic material properties.

A pure Lagrangian analysis of this problem does not run to completion because of excessive distortion in several elements, as shown in Figure 2. The contact surface cannot be treated correctly because of the gross distortion of the elements at the troughs of the sinusoidal rigid surface.

Figure 2. Eventually, the purely Lagrangian analysis will terminate because of excessive element distortion.

Adaptive meshing allows the problem to run to completion. A Lagrangian adaptive mesh domain is created for the entire blank. Abaqus/Explicit automatically chooses suitable defaults for adaptive meshing; hence, the adaptive mesh approach requires only two additional input lines:

HEADING
 ...
ELSET, ELSET=BLANK
***************************
STEP
DYNAMIC, EXPLICIT
 ...
ADAPTIVE MESH, ELSET=BLANK
 ...
END STEP

Figure 3 and Figure 4 show the deformed mesh at various stages of the forming analysis. Because the mesh refinement is maintained on the areas of the secondary surface that contact the die troughs as the material flows radially, contact conditions are resolved correctly throughout the analysis.

Figure 3. Deformed configuration at an intermediate stage of the analysis.

Figure 4. Deformed configuration upon completion of the analysis.

This example shows how adaptive meshing can be used in a steady-state simulation to allow the flow of material through Eulerian boundaries on the problem domain. A steel plate is passed through a symmetric roll stand to reduce its height by 50%. This simulation is run until it reaches steady-state conditions.

Figure 5 and Figure 6 show the initial and final (steady-state) configurations in a purely Lagrangian model of this problem.

Figure 5. The initial configuration of the roller and the undeformed blank in the pure Lagrangian model.

Figure 6. The final steady-state configuration in the pure Lagrangian model.

Figure 7 shows this problem modeled using an Eulerian adaptive mesh domain, where material flows through the mesh.

Figure 7. The initial Eulerian adaptive mesh domain.

Only the region near the roller is modeled. The exact location of the free surface does not need to be known to set up the problem: it is created in a likely location, and the final steady-state position is found as part of the solution. Although not shown, a focused mesh can be used to capture steep strain gradients directly beneath the roller. The Eulerian domain reaches the same steady-state solution as obtained with the Lagrangian approach.

The Eulerian adaptive mesh domain is created by defining an inflow and an outflow boundary on the adaptive mesh domain. Adaptive mesh constraints are applied normal to these boundaries so that material will flow through the mesh (see Defining ALE Adaptive Mesh Domains in Abaqus/Explicit). Frictional contact between the roller and the blank pulls material through the adaptive mesh domain.

The problem is set up by making the following modifications to the input file for the pure Lagrangian analysis:

HEADING
 ...
ELSET, ELSET=BILLET
 ...
ELSET, ELSET=INFLOW
 ...
ELSET, ELSET=OUTFLOW
 ...
NSET, NSET=INFLOW
 ...
NSET, NSET=OUTFLOW
 ...
SURFACE, NAME=INFLOW, REGION TYPE=EULERIAN
 INFLOW, S1
SURFACE, NAME=OUTFLOW, REGION TYPE=EULERIAN
 OUTFLOW, S2
***************************
STEP
DYNAMIC, EXPLICIT
Data line to specify the time period of the step
 ...
ADAPTIVE MESH, ELSET=BILLET, CONTROLS=ADAPT
ADAPTIVE MESH CONTROLS, NAME=ADAPT
ADAPTIVE MESH CONSTRAINT, TYPE=DISPLACEMENT
 INFLOW, 1, 1, 0.0
 100, 2, 2, 0.0
 OUTFLOW, 1, 1, 0.0
 ...
END STEP

Adaptive mesh controls were not required to solve this problem; they were included for illustrative purposes (see ALE Adaptive Meshing and Remapping in Abaqus/Explicit for details).